Frontal Crash Simulation on NEON Car Model

Aim-

• To perform the frontal crash on Neon car model and study about deformation and stresses developed and energy distribution in the car components.

 

Objective-

• First to check the unit system.
• Create type-7 contact with friction value 0.2 with recommended parameters.
• To check for penetration and intersections in the model if present.
• Check for the rigid body if any means make sure all components are connected properly.
• Create a planer rigid wall with a 0.1 friction value.
• Add mass on the given body to reach the target of 700kg and make COG align approximately with the seat rail.
• Give an initial velocity of 35mph(mile per hour) which is 15.6464 m/s in the x-direction.
• Give time step of 0.0001 for Brick Noda and Inter.
• Give the run time of 80 ms in the run card.

Request for additional TH output-

• Sectional force in the rails at the location of indicated node 174247.
• The axial force received on the rails from the bumper.
• Shotgun cross-sectional forces.
• A pillar cross-section.
• Acceleration curve received on the accelerometer at base of B pillar (on B pillar rocker).
• Intrusions on the dash wall 66695,66244.

 

 Theory:

A crash test is a virtual reconstruction that replicates the same force and speed that would occur if the vehicle was to be involved in an actual crash. In this type of testing, since nothing is physically impacting the body-in-white (BIW), no physical deformation or damage occurs to the body's structure, allowing multiple crashworthiness tests to conduct in succession.

• Frontal crash test.
• Side-impact crash test.
• Roof crash test.

Since in frontal crash test, there are multiple standards used on which we have to focus.

FMVSS 208-

• Federal Motor Vehicle Safety Standard 208 (FMVSS 208) regulates automotive occupant crash protection in the United States. Like all other Federal Motor Vehicle Safety Standards, FMVSS 208 is administered by the United States Department of Transportation's National Highway Traffic Safety Administration.
• This test procedure is used to determine whether a vehicle meets the conditions, requirements, and injury criteria specified in Federal motor vehicle safety standard (FMVSS) No. 208, Occupant crash protection.
• In this test, according to FMVSS 208, we give the initial velocity of 35mph(mile per hour)or 15.56m/s to the Car body.

Euro NCAP-

• Euro NCAP tests cars against a rigid barrier with full overlap at a test speed of 50 km/h. A small female frontal impact dummy is seated in the front driver’s seat and in the rear passenger side seat.

• In this, we perform crash and we give initial velocity as 35mph(mile per hour).
• This test places high demands on the restraint systems in front and rears seating positions. Strict limits are placed on the decelerations of the chest and on the degree of chest deflection and this, in turn, encourages manufacturers to fit more sophisticated restraints.
• The test complements the offset deformable test as a balance must be found between a restraint system that is stiff enough to restrain a male dummy in the frontal offset test and one that is compliant enough not to put injuriously high deceleration forces on a small female.
• In this tets overall we make car structure stiffer, so it can help to reduce lower leg and head injury.

 

 

Procedure:

 

1. Import the model in hypermesh.

• Go to File> import>Import solver deck> select the file from the folder.
• Or, we can drag down(by shift+right click) the 0000.rad file and release on hypermesh GUI.

 

 

2. Check for units in Hypermeh:

Hypermesh

Go to Solver>cards>Begin card

 

 

 

3. Create type-7 interface contact with friction value as 0.2.

Go to create > INTER > Type-7

• Select all the recommended parameters for Type-7 contact.
• Select all the components in slave and master as well to give self contact.

 

4. Check for initial penetration and intersection.

• Here we will check for initial penetration in the model.

For that go to tool > Penetration check > Select group > Check

 

• After selecting, groups, hit on check it will show the result below.

• Here we can see that 0 collisions were found.

 

 

5. Create an Infinite plane rigid wall with friction 0.1.

Go to Create > RWall > Plane

• Click on the blue arrow it will allow selecting node manually on FE.
• After selecting node coordinates of a node will display as below.

• Now to move the rigid wall plane in the x-direction to give space between the rigid wall and car body.
• Manually put the value for x co-ordinate as 4600 so rigid will move approximately 12 mm.
• Also, give -1 normal in the x-direction to make rigid wall perpendicular from point of contact.
• The slide option gives a slide with friction with a friction value of 0.1. 

• Infinite planner Rigid wall created now

 

6. Perform mass balancing in hypermesh.

• For mass balancing first, we will check the initial mass of the model for that,
• Go to Tools > Mass details > Mass, It will show the initial mass as shown below as 188.4 kg.
• To reach the mass value of 700kg we need to add 511.6 kg mass more. 
• For mass addition, we will use the ADMAS option.

For Add mass

Go to Solver Browser > Create > ADMAS 

• We will choose type-1, which will distribute the mass over the nodes which we give as shown below.

 

 

• Similarly, we will add mass over the floor panel to reach 700kg mass. 
• And to place COG at the right place on the rail.
• Now we can see the COG location and target mass as 700 kg.

 

7. Give an initial velocity of 35mph or 15.6464 m/s.

Create > Boundary condition > INVEL 

 

• Now here in INVEL card give a velocity of 15.64 on the global x-axis.
• Select all components because we are going to give the initial velocity for the whole BIW parts.

 

 8. Give time step for Brick, Noda, and Inter as 0.0001 milliseconds with respective scale factors.

To give time step go to Model browser> cards > ENG_DT_BRICK

 

• Give CST type and add value for scale factor and time step.

 

• Similarly, we will do for NODA.
• But here we will give a scale factor of 0.67.

 

• Now we will give the time step for the interface and we will choose DEL here.
• DEL will activate the delete element command if the time step goes below the given time step.

 

 9. Create intrusion spring on dashboard position to measure the deformation.

• Here we will deploy an intrusion spring to measure the deformation.
• This means how much spring length will change, will tell the length of BIW deformed in the passenger compartment. 

Go to Geometry > Temp node > select nodes > add.

• Now deploy spring connection between nodes,

Go to 1D > Spring >Spring2 > Select nodes

• Create a different collector for this intrusion spring so that we can assign property for this spring.
• Now create a property card for intrusion spring.

• Select as P4 spring and mass value as 1gm and stiffness 1N/mm.

 

10. Create sections on the Shotgun, bumper, rails, and A-pillar.

• we are creating sections to analyze the amount of force is traveling from that region.

 

• Select nodes in a way that the frame z-axis should come perpendicular to the global coordinate system.

• The frame is created now.

 

Now after the frame, we will create a section,

 

• We can select the N1, N2, and N3 in the same way we selected the nodes for the frame.
• Then we can see the red blu and green arrows which is showing the section plane.
• Then in frame id select the frame which we have created earlier.
• Now select the elements in the region where we are going to create a section, for that right click on gshell_id and create and edit and select elements.
• Put the factors value of deltaT=0.001 and alpha=0.67.

• Hit on proceed and we can see the section is created successfully.

 

• Now similarly we will create frame and sections for the right shotgun, for rails according to the node id given, and for A-pillar and for the bumper as well.

 

11. Create Accelerometer

• We will request TH file for acceleration curve received on the accelerometer at base of B pillar (on B pillar rocker).'

For that First create an accelerometer,

 

• First, create the node on which we will deploy the accelerometer.
• Now in the below picture, we will select that node in node_ID and name this accelerometer as the right accelerometer.

• similarly, we will do for the left accelerometer as well.

 

 12. Output Request:

a). Now request for TH file for accelerometer

• Create a new card for the accelerometer TH file.
• Select both left and right accelerometers in Entity IDs.

 

b). Now request for TH file for Interface-

 

• Here we have only one type-7 contact (all other types of contact deleted already).
• So request for this only.

 

c). Now request for TH file for sections-

• Select all sections we had created.

 

d). Now request for TH file for intrusion spring-

 

 

Run the simulation:

• To run the simulation go to Analysis > Radioss.

• After clicking Radioss click on the input file and save it in a new folder as Test-1 as shown below figure.
• Check the include connectors and option as -nt 4.
• N indicated how many cores will involve to run the simulation.
• It will make simulation faster. 

• After that click on Radioss, it will start the simulation.
• And wait until the new window popup and show as Radioss job completed.
• After running the simulation we will get the animation file, h3d file, and also the T01 file.
• Check for all the files.
• Now open 0001.out file and check all the details. 
• Here we can see all variables in the out file about energy error and mass error also.
• So for checking the maximum loss check the last cycle details.

 

Here in the last cycle of the simulation, we have maximum energy losses where,

Energy error  = -1.8 %     Acceptable     (Range is -15% to +5%)

Mass Error     =  0           Acceptable     (Range is 0 to 2%)

So the resultant energies are,

1. Internal Energy       0.4145E+5
2. Kinetic Energy         0.4067E+5 
3. External work          -1611
4. No of cycles             418256

 

 

Result Plots-

• Review the simulation using Hyperview.
• Plot the graphs using Hypergraph-2D

 

1. Review the simulation using Hyperview.

Split the screen in two-part-

 

• Now after splitting the screen open hyper view after switching into in 2nd screen.

• In Hyper View, the window import the h3d file for a simulation run.

 

 

Animation-

• Now after importing the h3d file on hyper view GUI go for contour activation.
• In contour, it will show the simulation graphically and contour lines of load and other properties variation.
• To activate contour go to Toolbar > contour as shown below.
• Go to Contour > Displacement > apply contour.

 

 

 

• From the above simulation, we can see that the deformation is starting to take place from the bumper component. since this is the component that is coming in contact first. And here in bumper some amount of kinetic energy will get stored in internal energy as deformation take place.
• After that remaining Energy will transfer to further components which side rails and hence side rails start deforming and it will also absorb some amount of energy.
• Then Shotgun starts deforming with and it will also absorb some amount of energy then finally A-pillar will deform.
• So according to the above discussion, we can understand that all the impact should absorb within the front section means before the passenger compartment.
• Deformation we can see that is not proper and realistic means BIW is kind of going down is just because there no chassis and suspension and wheel system present in this model.

 

• similarly for Von-mises:

 

• Stress distribution over the model is quite good as we can see there are only a few regions in the bumper system that have stress concentration.
• Otherwise, stress is distributed all over the BIW model.

 

 

 Plot the graphs using Hypergraph-2D

• Now split the window in 3Part and open hypergraph-2D in the new window.
• After opening the hypergraph window import the T01 file in Hypergraph.

First, we will plot the graph which we have requested,

A). Section forces-

1. Bumper sections

• Since we know that the impact will come on the bumper first so forces will also come highest on the bumper.
• On both left and right bumper, forces will be the same approximately as shown below the graph.

• As we can see from the simulation that the bumper is coming first into contact with the rigid wall so the amount of force also will be more on the bumper that is 14.74KN on the left side of the bumper and 15.25KN on the right side of the bumper. 

 

2. Rail sections

• After bumper force will travel through rail. so the second component which comes in contact with the rigid wall will be the rail section. 

• The amount of force traveling by the left rail section is 21.85KN and 45.99KN from the right rail section.

 

3.shotgun sections-

• The shotgun section will be next after the rail section.

• From the graph, we can see that the value of force which should go through the shotgun section is approximately equal to the graph value.
• From left shotgun section 11.42KN and from right shotgun 8.82KN of force traveling.

 

4. A-Piller sections

• In the front crash, we should take care of one point that, least amount of force should travel from A-pillar to keep the passenger compartment safe.

• Which is displayed in the graph in left 9.1kN and in right 5.82kN.

 

 

B). Spring Elongation-

Spring elongation of spring with node id 66695:

• These intrusions of spring show that how much leg area of the passenger is safe.
• This means the spring should not be compressed more the 150mm of 15cm.
• according to the graph, we can see that the maximum intrusion is 100.66mm and 90.01mm respectively.  

 

Interface-

• This graph is showing the force generated due to self contact with respect to time.
• So the maximum amount of force-generating due to self contact is 134.88KN.

 

Accelerometer graph

• The accelerometer graph is showing the maximum acceleration received by the B-pillar section due to this crash.
• Since we had deployed accelerometer to both sides on the B-pillar base so there are two graphs which are showing both accelerometer values.

• In the left accelerometer, the amount of acceleration observed is 345.88 mm/ms^2 and on the right side, 227.54 mm/ms^2.
• These values are in an acceptable range.

 

Global Energies-

• Now we will study the energy variation throughout the simulation.
• Here is the cumulative graphical variation of all types of energies involved in the simulation.

 

Internal Energy-

• At time t=0 internal energy will be zero, and as impact begins the amount of force causing the stress due to which strain starts taking place and deformation happens.
• So due to deformation some internal energy will start storing within the body and keep increasing as deformation increases in the body.

 

kinetic Energy-

• Since we have given an initial velocity to the car body 0f 15.6464 m/s and car body itself has its mass so according to the kinetic energy formula.
• 1/2 mv^2 = 85241.8kJ(kilo joule)
• The value shown by the graph below is less than the calculated value is just because of energy error. 

 

Contact Energy-

• Contact energy is due to the self contact of FE elements of the car body.
• So according to the graph, the maximum value of contact energy is 1043.2KJ.

 

Hourglass Energy-

• Since we already used shell parameters, instead of that we observe some amount of hourglass energy.
• This hourglass happens in some region where goes below the given timestep due to stress concentration in the coarse mesh.
• For that, we particularly work on that region to refine the mesh.
• But here the value is 291.51KJ less than 10% of the internal energy value(10% of 41450 is 4145KJ).
• So this hourglass value is acceptable.

 

Total Energy-

• The total energy is the combination of all energies present here,
• The maximum value of total energy is found at 85241.8KJ.

 

 Result-

• Mass balancing is done for the given BIW for a final value of 700kg.
• Created Typ-7 Interface contact for BIW self contact.
• Created rigid wall with friction value as given.
• Timestep value is given for all types of elements and contacts.
• Initial velocity is also given to the BIW body.
• An intrusion spring is created to measure the deformation or to ensure safety for the passenger leg area.
• An accelerometer is installed at the base of the B-Pillar.
• All TH files are requested for output and then run the model checker.
• Run the simulation and post-processed in hyper view and hypergraph.

 

Learning Outcome-

• How to balance mass in the hyper crash and hypermesh.
• How to create a rigid wall for the frontal crash.
• How to create interface contact and set all the required parameters.
• How to give initial velocity and time step values for brick shell and interface.
• How to request for TH file which will be used in post-processing of the simulation.
• Learned how to create frames and sections to determine sectional forces and their importance.
• Get to know what are standards used for crash analysis like FMVSS, Euro-NCAP, etc.